1
\$\begingroup\$

I have added several pads with plated holes and assigned them to the GND net to serve the purpose of mounting holes for my PCB. I'd like to create a Design Rule for them which connects them to a GND polygon without thermal relief (direct connect). I assigned a Designator of H to them to differentiate them from other pads, thinking that I could write a simple query to target only pads with this designator.

Scouring the query builder/helper and documentation, selecting pads by their designator seems like an impossible task. There is no parameter, field, or property in the query language that appears to select pads by the value assigned to their designator.

There is a Name parameter, but writing syntax like (Name = 'H') doesn't select the pads.

Is there a way to select pads with a specific designator using the query language in Altium?

\$\endgroup\$
1
  • \$\begingroup\$ Free pads for test point access might also be worth discussing, since they have a similar solution. \$\endgroup\$ Sep 27, 2023 at 4:21

1 Answer 1

1
\$\begingroup\$

Pads can be confusing without knowing that Altium Designer prepends their parent component designator to create the Name property. For example, if a component with designator CN1 has a pad with designator 3, its name will be CN1-3.

This is somewhat discoverable by using the PCB panel to select specific elements. (Select Pad & Via Templates, then <Pads>, and browse through the resulting list.) Here, you can see that the selected pad (in this case, pad 3 within CN1) shows its name just before the coordinates. (Note also that this component has some pads without designators, which appear as CN1-.)

PCB panel in Altium showing pad selection

Pads that are added to the PCB directly do not belong to a specific component, and Altium assigns them the parent "component" of Free. Thus, pads without designators will appear in this list simply as Free-:

PCB panel showing selected free pad without designator

If you assign such free pads a designator, such as H, they will be given the name Free-H:

PCB panel showing selected free pad with designator

Armed with this information, you can create a query or Design Rule like the following that will target them:

IsPad AND (Name = 'Free-H')

The documentation talks about such pads being referred to as "free" pads but I was never able to find anything that explains this naming mechanism.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.